FEA Postprocessing of a Flat Head with Internal Ribs - ASME BPCV Sec VIII Div 2 Part 5 1

[az5333]

Hi Fellow Senior Engineers. I am working on evaluating a pressure vessel made out of Cast Iron (SA-278 Cl 35) material. I have performed the analysis for evaluating thickness of the shell using ASME Sec VIII Div 1. However, since the head is flat with internal ribs (please see attached pics for reference) and Div. 1 does not provide guidance on such a design, I am using Div 2 Part 5 to evaluate the acceptability of the head usign Desing by Analysis approach. I have done the FEA using SimScale and now I am trying to post-process the data using Paraview as per Div 2 5.2.2 (Elastic Stress Analysis Method). I have created an SCL using Paraview and I have the 6 Cauchy stress tensors. I am unsure about how to calculate the membrane stresses and corresponding principal stresses to compute equivalent Von Mises Membrane Stress. I am also attaching the snapshot of the excel data I have so far. Can you please guide me if I am going the right direction and how to proceed forward. Many thanks.

 

[az5333]

Attached is the pic of the flat head.

 

[TGS4]

Do you understand how to linearize the component stresses, based on the through-thickness distribution that you have extracted? Do that (refer to 5-A.4.1.2). Graphing it really helps. From there, with the 3x3 matrix of membrane stresses, calculate the principal stresses. For the membrane-plus-bending, please make sure to follow the direction given in 5-A.4.1.2, Step 2(a).

I note that your normal stresses are mostly compressive. You will need to check for buckling.

And given the brittle nature of the material, I would seriously consider using the elastic-plastic method for demonstrating Protection Against Local Failure.

 

[az5333]

Hello TGS4. Thank you very much for your response. I have been following your posts very thoroughly in other forums as well. I am using the attached formula as pointed out by Prex in another forum for calculating Membrane and Bending Stresses considering equal nodal spacing. When calculating the membrane stress for each of the stress tensor components, can I use the default FEA output Cauchy xx,yy,zz components for the matrix or do I need to re-arrange them into the normal, hoop and meridonial stresses and then calculate principle stress? Does it matter? Sorry for asking such a trivial question.I am asking because in one of the excel sheets provided by PVEng for stress linearization, they had rearranged these components. thank you!

 

[TGS4]

The order doesn't matter. But don't miss the forest for the trees here. With the compressive stresses, you may be dealing with a buckling failure mode, and with the brittle material, you also need to seriously consider Local Failure.

 

[az5333]

Thanks TGS4. The only reason I was asking about the order is because of 5-A.4.1.2 states that "The component stresses used for the calculations shall be based on a local coordinate system defined by
the orientation of the SCL, see Figure 5-A.2.". So I was not sure what this meant and I need to change the coordinate system to Local or stay with the FEA Global coordinate system I used for the model.

Yes I will definitely take your advise and look at the buckling failure mode and local failure. I hope they are fairly simple procedures than the Linearization method

 

[TGS4]

Be aware that the Code Buckling analysis has issues. The better approach (and will be published in the Code in the 2023 Edition) is described in the paper Buckling of Cylinders due to External Pressure: Experimental Work Compared With Finite Element Stress Analysis.

I'm not sure that the procedure is easier - does your FE software do elastic-plastic analysis?

 

[az5333]

Thanks TGS4. I will go through the attached paper for buckling analysis. I am using Simscale. It does have an ability to do elastic-plastic analysis, but for cast iron I do not have data to create a true stress-strain curve as per Annex 3-D (since I think it is a brittle material?). I could not find any yield strength values in ASME Sec II against temperature. Please guide me in the right direction if I am not. Thanks again!

 

[TGS4]

Ummm - is SA-278 permitted in Section VIII, Division 1 construction? It appears to be only permitted in Section IV construction.

 

[az5333]

Yes, as per ASME Sec VIII Div 1 UCI-23 it is permitted but the allowable stresses are very low. These materials have bene used by the steam drum manufacturers for drying operations.

 

[az5333]

Hi TGS4. I am trying to check the following local failure criteria for the subject vessel, which asks us to sum the local primary membrane plus bending stresses for checking this criterion:

(σ1+σ2+σ3)≤ 4S.

My question is, previously we calculated membrane and bending stresses (which was one stress tensor per SCL) and then compared the Von Mises accordingly. Now for checking the local failure criteria at EACH POINT, how do I find the membrane and bending stresses for each point? Should I just find one Primary membrane stress tensor and one Bending stress tensor for the WHOLE cross-section of my vessel? Appreciate the clarification please.

 

[TGS4]

Use the elastic-plastic method for Local Failure, as I recommended earlier. I cannot endorse the elastic method in your situation.

 

[az5333]

Thanks TGS4 for your valuable inputs. OA couple more questions I am struggling with:
1. when considering load conditions for elastic analysis (as per Table 5.3 VIII Div. 2), is it expecting me to only consider pressure load and not consider temperature for design load conditions to compute Pm, PL and Pb? How do I calculate Q? Is it by just applying temperature to the pressure vessel and looking at the stresses?
2. Secondly, if I have 4 load cases to analyze the stresses, do I need to calculate Pm for all 4 load cases individually and then add (on a component bases) each of the Pm stress tensors for all 4 cases together to make a single Pm stress tensor and then evaluate it against the allowable values?

 

[sameer21101970]

i am new to PV design.
I have confusion in calculating membrane, bending stress & principal stress from excel file you have give.
will you please show single calculation. thankyou in advance.

 

[az5333]

Hi Sameer21101970. What confusion do you have? Will you please share the method you are using?

 

[sameer21101970]

Hello, thanks for your prompt attention.
I have taken your N data and want to calculate N_membrane.
I am following below procedure as per formula screenshot given in above discussion.

for
i=0 , dx/dt=1/2n & i=n , dx/dt=1/n for membrane stress
here n =11
so,
N0 = -833.28 = -833.28/2x11 = -37.8763
N1 = -933.53 = -933.53/1x11 = -84.866
N2 = -677.41 = -677.41/1x11 = -73.41
n3 = -529.13 = -529.13/1x11 = -61.58
like this upto N=11 and then Summation of all above.

Above procedure is correct of calculation of membrane stress.

Regarding Hand Calculating BEnding Stress, Principal stress. I request if you can show such basic calculation.

 

[sameer21101970]

Hello, Waiting for your reply.